Overcut support on CandCNC Ethercut

[whiskeymike]

I'm looking to stop divots from occurring in my cuts and I've read several threads here about using the overcut feature of Sheetcam to turn off the torch as it's ending a cut and have read that CandCNC Ethercut didn't support turning the torch off via this method because of time lag. But then read that an experimental firmware was made available to support it. Has anyone used this? Is it now available in the latest firmware generally available? I posted on the CandCNC forum yesterday but didn't see a response the website is down now, so I thought i'd ask here for experience as I want to implement this weekend.

Fyi, I found these two videos to be very helpful on rules for applying this type of thing.

https://www.youtube.com/watch?v=_gsNhcWF2lE
https://www.youtube.com/watch?v=hC_TRbmlzpE Couple mins in, it get's to the rules

[Diesel]

I'm also hoping that there will be a good fix/patch to allow this functionality since I'm experiencing divots at the ends of my cuts. Turning the torch off before the end of the cut seems to be the tip I see most often when folks are working through this issue.

FYI (my bad if you've seen this before):
If you want to send or post a link for a YouTube video and have it start at a certain point in the clip, there's a neat way to do it.

YouTube.jpg (45.06 KiB) Viewed 6778 times

YouTube.jpg (45.06 KiB) Viewed 6778 times

The resultant link that is produced just adds the "?t=2m11s" to the URL - so you could add it to a link after the fact if you're so inclined.
https://youtu.be/hC_TRbmlzpE?t=2m11s

Cheers,

Matt

[BTA Plasma]

Short arc leadout with overcut works perfectly on a very high percentage of geometry. Turning the torch off would be a feature for a single line cut and not necessarily be an advantage for any other geometry.

[exapprentice]

Hi whiskeymike

Is this the grail for the ethercut system
I like many others who purchased the ethercut would like to be able to stop divots at the end of an open line cuts, yes I agree with BTA Plasma
But surely its only when you cut "a single line cut" that you get the divot, it’s the only place using my ethercut that I can’t stop them from happening.

So with fingers crossed this could be a solution

Whiskey mike I’m with you just need to sort it out somehow, let’s hope someone who has greater experience chips in with some guidance on the best way to utilise the new CandCNCPlasmaRev11m1 POST via SheetCam

Best regards to all

exapprentice

[beefy]

There's quite a big thread on this matter which I started on the Candcnc forum.

The thread ended with Tom saying there was no solution (last time I checked which was quite a few weeks ago).

However, I came across another thread somewhere where Tom said he had found a fix. So I went back to the thread I started but there was no announcement there that it had been fixed. Nor could I find anything else on the Candcnc forum announcing a fix.

You are definitely going to have to get this info from the horses mouth. It's possible there has been an announcement since I was last on the forum. If there has been a fix, I wonder if it works on existing systems or only if it's an actual hardware fix.

The issue was related to the fast laser M10/11 command. That command is high speed and was designed for laser cutters. The Mach3 parallel port systems seem to work fine with it but the Smoothstepper board introduced latency issues.

Having read quite a few posts on hole cutting and getting the divot at the end of the cut, it seems the "divotless" success stories had a slight overcut and switched the torch off just before the end of the cut path (using the laser M10/11 command in gcode). I don't think they used any leadout. Search for "divot" here and you will see a thread or two talking about this issue.

Keith.

[Diesel]

There's a new update on CandCNC's site...perhaps this is the fix we've been waiting for?

https://www.candcnc.net/index.php/downloads

"EtherCut Updater 09/20/15
Download, Unzip and run the installer. It will update the HUB ADMIN Utitlity, the MACH plugins and copy the new DTHCIV device firmware version 1.9 to your C drive. This is for users that have either run the previous EtherCut Updater OR the Master Installer X. You should be on HUB firmware 1.6 and DTHCIV Device firmware 1.6 or 1.7
You MUST use the Hub Admin to apply the new firmware for the DTHCIV"

[dhelfter]

Updates are great, but there are hundreds of these systems working with the current firmware. That is not to say new better features and performance are not present, but if Dthc is not working now I highly doubt updating firmware is going to make it work.
I am also confused but everyone's excitement over being able to turn torch off before stopping motion. I completely see it with straight line cutting, but with a profile just increase the lead out? Maybe I am missing something.
Matt, I would really like to help you get the Dthc working. Send me an email, with the gcode and description of what is happening. Again we alone have over 50 machines out there with Dthc firmware 1.6.
If by putting a very large lead out you still get a divot, I suspect the divot is happening at the star of the cut, not the end.

Dan
Ldr

[Diesel]

Updates are great, but there are hundreds of these systems working with the current firmware. That is not to say new better features and performance are not present, but if Dthc is not working now I highly doubt updating firmware is going to make it work.
I am also confused but everyone's excitement over being able to turn torch off before stopping motion. I completely see it with straight line cutting, but with a profile just increase the lead out? Maybe I am missing something.
Matt, I would really like to help you get the Dthc working. Send me an email, with the gcode and description of what is happening. Again we alone have over 50 machines out there with Dthc firmware 1.6.

Dan
Ldr

I think folks are getting a little desperate since many upgraded to the 'latest and greatest' hardware (from the tried and true LPT port solution) only to have setbacks.

Well, everything I've seen out of 'ole Jim Colt as of late says to turn the torch off .xxx" before stopping motion. Without doing this, the arc is not fully extinguished by the time the end of the cut is reached and some systems may have more latency than others. Ether-Cut's latency issues might be exaggerating this.

Methinks Jim's advice is rooted in the parameters that make the Hypertherm True Hole technology possible. It's not an apples:apples comparison, though. That isn't traditional air plasma and they have some $$$ software in play that effectively makes critical tool path decisions for the operator. That said, what he's suggesting seems to make sense on paper...but I'm so new with plasma that I can't comment on that with any authority.

Thanks, Dan.
I know we'll get it working and I appreciate your efforts.
More than anything, I'm here posting this because I've seen so many others with eerily similar issues. What I learn can be used to help others.

Cheers,

Matt

[Diesel]

If by putting a very large lead out you still get a divot, I suspect the divot is happening at the star of the cut, not the end.

I'll have to give that a whirl. I haven't tried any lead outs bigger than .2"

Cheers,

Matt

[beefy]

Updates are great, but there are hundreds of these systems working with the current firmware. That is not to say new better features and performance are not present, but if Dthc is not working now I highly doubt updating firmware is going to make it work.
I am also confused but everyone's excitement over being able to turn torch off before stopping motion. I completely see it with straight line cutting, but with a profile just increase the lead out? Maybe I am missing something.
Matt, I would really like to help you get the Dthc working. Send me an email, with the gcode and description of what is happening. Again we alone have over 50 machines out there with Dthc firmware 1.6.
If by putting a very large lead out you still get a divot, I suspect the divot is happening at the star of the cut, not the end.

Dan
Ldr

Don't understand the comment about firmware not fixing things. A great many pieces of equipment use programmed ICs, and firmware revisions fix all sorts of problems.

No one stated the ethernet system is "not working", it simply has (had ???) ONE known flaw in that it couldn't take advantage of the fast M10/11 laser commands which is what is needed to turn the torch off with good position accuracy during motion. Apart from that one single problem I've heard nothing but good things about the ethernet system.

From what I have read, "everyones excitement over being able to turn torch off before stopping motion" has been related to HOLE CUTTING, not general profiles. Lots of guys want to be able to cut great looking holes, especially if the job is for a customer. People have tried various attacks to prevent the divot at the end of cut, and the ones with good success seems to have been a mixture of overcut and ACCURATELY (which required the M10/11 commands) switching the torch off just before the end of the travel path. Seemed even leadouts could be problematic because when cutting holes the slug can immediately fall out then then "flame" is searching for metal and causes the divot. If you have any recommendation on how to get divotless holes without the aforementioned techniques, then let's see if anyone can use them and the get the same results. The more strings we have to our bows the better.

If you have a smooth lead in then what could cause that to create a divot at the start of the cut ?? There'd have to be a pause in motion at the start of the cut or something like that. Or perhaps a perpendicular lead in is being used and there's poor accel/decel at the corner of the cut. However the guys who have been striving for these great quality holes (like SeanP) are not beginners to this game. I'm sure they would have noticed if a divot was happening at the beginning of a cut.

Keith.

[beefy]

Methinks Jim's advice is rooted in the parameters that make the Hypertherm True Hole technology possible. It's not an apples:apples comparison, though. That isn't traditional air plasma and they have some $$$ software in play that effectively makes critical tool path decisions for the operator. That said, what he's suggesting seems to make sense on paper...but I'm so new with plasma that I can't comment on that with any authority.
Matt

Hi Matt,

most of Jims suggestions are what can be applied to our basic air plasma IF the cnc software / hardware can implement it (like the mentioned M10/11 commands). Jim does tend to differentiate about what can and can't be achieved with our basic systems vs the higher end ones.

Keith.

[Diesel]

I think Dan's comments mostly centered on the fact that there are lots of folks out there with Ether-Cut (and DTHC-IV) not having any issues.
Then there's me...and others...that are having issues.

Most of Jims suggestions are what can be applied to our basic air plasma IF the cnc software / hardware can implement it (like the mentioned M10/11 commands). Jim does tend to differentiate about what can and can't be achieved with our basic systems vs the higher end ones.

I agree.
Thanks for the clarification.

Cheers,

Matt

[exapprentice]

Hi Guys

I am relatively new to pllasma cutting but that is not say I havent struggled at times from the start of building my own table from sctratch
In my nievetey I went with the ethercut MP3500 at the time as it seemed to give the best options.
I am more than happy with the results to date and how it all ties in (apart from the painful lesson of what happens if you try running it all to fast)

My only issue is with open line cuts (which feature in some of the parts I cut) and the divots at the start and end of the lines, closed shapes seem good and seem to cut OK

I am thinking about trying the ramp option for the lead ins but no matter what I tried at the end I still ended up with a divot to varying degrees at the end
I have also tried negative values for the overcut but les at sheetcam says that will only be effective on closed shapes

Its Great to read a mature thread regarding the Ethercut system, I have done the upgrades as and when available and as I have said more than happy with the whole set up apart from the "open Line" divots

Apperently the new POST (CandCNCplasmarev11M1) has the options of using M10/M11 + M03/M05 also additionally M10P1 (quick torch off) which can be writteninto a rule the only really unkown (assuming the off commands work as they should is going to be where/at what distance before the end of cut (open line) do you place the rule
I am sure if all those that have read this post stick together on this we will all benifit in the long run, I assume thats why we are all reading and contributing to help each other

sorry its a bit of a rant just thinking and typing at the same time
Best regards to all
exapprentice

[dhelfter]

Sorry I came across like firmware doesnt fix anything.
Reread my post, and sure enough that is how it sounds.

What I was commenting toward was more directed at one of our customers, Diesel. He said he has to cut with dthc off (sorry may be in another thread). I was just suggesting there is no reason he should (except of course something is wrong!) and I really want to help him get it working correctly! All I was saying is I do know dthc will work with firmware version 1.6.

I will post some pictures later (when I get to shop) of parts we have cut and settings used.

Dan
LDR

[exapprentice]

Hi dhelfter

I have updated my firmware for the DTHCIV to the latest rev 1.9all seems good and runs as it should

its this latest revision that lets you use the codes I wrote about above, which if "we-collectively" can work out the finer details.
As I have already said I am quite new to plasma cutting but I am sure someone who understands rules and has far greater expieriance of using
sheetcam with the ethercut will drop some of us some clues on how to dial it in to optimise the latest update.

best regards to all
exapprentice

[whiskeymike]

FWIW, I posted a question about this on CandCNC's forum and received a response about the firmware being available and a bit of information on how to use it. It flew over my head, so if anyone tries it out and get's it working, please post a note on what neophytes like myself are supposed to do.

http://www.candcnc.net/supportforum/vie ... ?f=8&t=968

My next step is to make sure I've got the latest firmware loaded and then look at the post rules. But I'm not sure how to determine the distance piece that was referred to in the thread.

[Diesel]

I updated to the latest v1.9 firmware this afternoon.
I still haven't experimented with the overcut functionality yet.

I just registered for the CandCNC forum site...so I can't check out that link just yet.

Cheers,

Matt

[exapprentice]

Hi everyone

Has anybody tried using the new CandCNCPlasmaRev11M1 post yet

I am getting an error message when I go to post process

I thought I would try and dial in some numbers to turn the torch of before the end of cut to post the results on here
but obviously not able to at the moment

Best regards to all

exapprentice

[WyoGreen]

I have loaded the 11m post. There is an error in the post, if you go to the line that the error referenced, you will find an IF Then line, the Then comment is one line down from where it should be. I can't remember the line number now, it seems like it was 532? or there abouts. If you post your error line number, I will go to that line and take a screen shot of what it should be.

Steve

[exapprentice]

Hi Steve

thanks, I have issues with the new POST, I get the following error message:
"An unexpected error has occurred
Post not found
This error occurred on line 1178 in file ..\camlib\postmacro.cpp
Post processing failed"

I also see the following message in sheetcam under machine options/select post processor/CandCNCPlasmaRev11M1 POST
In the text box is the following message:

Lua: Syntax error during pre-compilation
… ..... \appData\roaming\SheetCam TNG\posts\CandCNCplasma-rev11M1.scpost:508:
‘then expected near ‘post’

Has anyone any idea what thet means??

Best regards to all
exapprentice

[Diesel]

I get an error message very similar to that when I attempt to re-post the same g-code file (.tap) that is currently loaded in Mach.
I've since learned to close the currently loaded g-code in Mach before attempting to repost the same code/file in SheetCAM.

Your syntax error sounds like you have some code out of place in the post.

Cheers,

Matt

[WyoGreen]

exapprentice, the attached .jpg shows how line 507 and 508 should look. If I remember right, the "then" in line 507 was on line 508.
If you correct that, the post should compile all right, and that should cure your other error when you try to post to g code.

OnPenUP.JPG (60.98 KiB) Viewed 6558 times

OnPenUP.JPG (60.98 KiB) Viewed 6558 times

Steve

[exapprentice]

Hi Steve

Thank you for your help, I will look into the code and attempt to correct the error, fingers crosed I hope it works

Thanks again for your help in sorting this bit out

Best regards to all

Peter

[jimcolt]

Most high end industrial quality (and price) CAM Nesting software has the ability today to automatically modify files with proper "overburns" and "negative cut-off" at the end of each cut cycle. An overburn Is simply going slight past the lead -in kerf, but staying on the original path of the cut, Negative Cut-Off (these functions go by different names on different brand softwares) is timing that allows the plasma arc to shut off before the torch reaches the end of the overburn.

When cutting steel with an air plasma (or an oxygen plasma) the torch continues burning after the DC power is shut off. This is because the gas flow continues...and the exothermic (burning) of the steel is supported by the air flow (it is the 20% oxygen content that created the exothermic reaction). So.....if you stop the motion and the plasma at the same time....the torch sits in one place and burns a divot.

The idea of the combined overburn and negative cutoff is to keep the torch moving while it is slowly extinguishing (maybe 30 miliseconds) the exothermic reaction. When the timing is exactly right...the exothermic reaction extinguishes just at the lead-in kerf crossing point on your hole (or whatever shape you are cutting) and planes off any tabs that may have been left there.

We actually had been modifying machine code for years with CAM software....however the timing is extremely critical, different timing is also required for every different material thickness and power level as well. Ultimately developing the True Hole process was a 3 year engineering effort that involved cutting hundreds of thousands of different diameter and thickness holes, and developing a data base to support it. Further....taper was removed by introducing a pure oxygen shield gas that made the oxygen cutting arc very aggressive (only works on holes, only works on Hypertherm's HPRXD plasma systems)....which required even more data and technology that allows automatic and rapid switching of shield gas from air to oxygen and back to air again. True hole is a very robust process on high end machines ....but is very complicated, and contrary to popular belief....is not all "smoke and mirrors" in the CAM software! (some competitors like to say that about the technology!)

So, I have actually been able to almost get rid of hole divots on my Plasmacam by experimenting with no lead out....and leaving a gap at the end of a circle (before 360 degrees). again the timing and the dimensions are critical.....but work repeatedly as long as you use the same gap, same amperage, same cut speed, etc.

Jim Colt Hypertherm

[whiskeymike]

Thanks Jim. So you leave a small ~.01" gap (which varies by thickness of material) in the dxf drawing and that basically accomplishes a similar scenario. Makes sense. I'll try it on a few things this weekend.

If I can get rid of the divots, I think it'll really add to the overall quality of my pieces. The divots are the only thing at the moment that I don't like.